Hi, I would like to save durin
 

Hi, I would like to save during the run time, data (and cells) that intersect a plane. I saw the cuttingPlane class, but is there a code snippet on the web showing how to save those cells in a top level solver?
I want later on to be able to read those files with paraFoam or paraview.

Dragos

Hi Dragos, yes, check this th
 

Hi Dragos,
yes, check this thread. In case you need further
advice please continue the thread and I'll help
you. The cutting plane is very practical if you
like to take your data to matlab, gnuplot etc for
further analysis.

http://www.cfd-online.com/OpenFOAM_D...tml?1197913395

best regards,
Ville

Hi Ville, Actually your answe
 

Hi Ville,
Actually your answer was the source of my information in the first place. There you show how to access the cells and data, but I am interested in saving them in openfoam format. Can you show me how to do that?
If you help me, I promise to put toghether a wiki page so other people would benefit from it.

Dragos

Hi, unfortunately I doubt if
 

Hi,
unfortunately I doubt if that is possible since
the cutting plane option is needed to extract data from the mesh so that connectivity information (which the post processor should need) is lost..
-Ville

Get the cells from the cutting
 

Get the cells from the cutting plane and construct a cellSet from them. Something like

const labelList& cutCells = cutPlane.cells();

cellSet someCells(mesh, "someCells", cutCells);

someCells.write();

Then use foamToVTK with -cellSet option.

Thanks both of you! This is w
 

Thanks both of you!
This is what I was after.

...me again. The following co
 

...me again.
The following code works very well:

point pnt(0.5,0.25,-0.25);
vector direction(1,0,0);
plane pl1(pnt,direction);
cuttingPlane cutPlane(mesh,pl1);
const labelList& cutCells = cutPlane.cells();
cellSet someCells(mesh, "someCells", cutCells);
someCells.write();


Here is a slice obtained with it:
http://www.cfd-online.com/OpenFOAM_D...ges/1/6528.png
... but I would like more. Is it possible to save together with the above cell set also the data associated to it at a certain time?

Dragos

Hi Dragos Thanks for the co
 

Hi Dragos

Thanks for the code.

Could you also please post the list of include files so that this code compiles successfully. I put the code in my post processing routine exactly as you have psoted


point pnt(0.0,0.0,0.04);
vector direction(1,0,0);
plane pl1(pnt,direction);
cuttingPlane cutPlane(mesh,pl1);
const labelList& cutCells = cutPlane.cells();
cellSet someCells(mesh, "someCells", cutCells);
someCells.write();

and get the following error:

postProcessing.C:654: error: 'plane' was not declared in this scope
postProcessing.C:654: error: expected `;' before 'pl1'
postProcessing.C:655: error: 'cuttingPlane' was not declared in this scope
postProcessing.C:655: error: expected `;' before 'cutPlane'
postProcessing.C:656: error: 'cutPlane' was not declared in this scope
postProcessing.C:657: error: 'cellSet' was not declared in this scope
postProcessing.C:657: error: expected `;' before 'someCells'
postProcessing.C:658: error: 'someCells' was not declared in this scope
postProcessing.C:656: warning: unused variable 'cutCells'


The list of files I have already included are:

#include "fvCFD.H"
#include "wallFvPatch.H"
#include "interfaceProperties.H"
#include "twoPhaseMixture.H"
#include "incompressible/turbulenceModel/turbulenceModel.H"
#include "nearWallDist.H"
#include "fixedValuePointPatchFields.H"


Thanks alot

With Kind Regards
Jaswinder

Hi Dragos I just checked o
 

Hi Dragos

I just checked out the cuttingPlane code and it has a member function called


//- Sample the cell field
template<class>
tmp<field<type> > sample(const Field<type>&) const;

It seems that if you add the following to your code snippet

point pnt(0.0,0.0,0.04);
vector direction(1,0,0);
plane pl1(pnt,direction);
cuttingPlane cutPlane(mesh,pl1);
const labelList& cutCells = cutPlane.cells();

----------------
volScalarField slicedDesiredField = cutPlane.sample(desiredField);
-----------------

cellSet someCells(mesh, "someCells", cutCells);
someCells.write();

You might be able to extract the field you want.

I could not test whether if it works as i am unable to compile the original code offered by you.

With Kind Regards
Jaswinder

Hi Dragos I have solved the
 

Hi Dragos

I have solved the compilation problem but now I have problem visualizing it.

I give the following command:

foamToVTK <root> <case> -cellSet someCells

and it writes


Exec : foamToVTK . 7_flask_10ml_320rpm -cellSet someCells
Date : Jan 30 2008
Time : 17:48:12
Host : taifun
PID : 5343
Root : <root>
Case : <case>
Nprocs : 1
Create time

Number of cells in new mesh : 6034
Number of faces in new mesh : 24264
Number of points in new mesh: 12342


--> FOAM FATAL IO ERROR : cannot open file

file: /scratch1/power_consumption_sims/1st_10ml/7_flask_10ml_320rpm/system/subsetSubse t/fvSchemes at line 0.

From function regIOobject::readStream(const word&)
in file db/regIOobject/regIOobjectRead.C at line 66.

FOAM exiting


Could you please give me a clue what is missing

With kind Regards
Jaswinder

Hi Jaswinder, Thanks for the
 

Hi Jaswinder,
Thanks for the information, I'll definitely try it (I have to check if volScalarField class can write down the data). On the other hand I have no idea why you get that error.

Dragos

foamToVTK .. cavity -cellSet c
 

foamToVTK .. cavity -cellSet c0

works for me (1.4.1):

Time constant

Internal : "../cavity/VTK/c0_0.vtk"
Original cells:5 points:24 Additional cells:0 additional points:0

Patch : "../cavity/VTK/movingWall/c0_0.vtk"
Patch : "../cavity/VTK/fixedWalls/c0_0.vtk"
Patch : "../cavity/VTK/frontAndBack/c0_0.vtk"
Patch : "../cavity/VTK/oldInternalFaces/c0_0.vtk"

Hi Mattijs, Will you give me
 

Hi Mattijs,
Will you give me a clue on how to get only the slice (both geometry and data)? I don't want to save the entire domain and then to get the slice.

Dragos

pull out the bits of code from
 

pull out the bits of code from subsetMesh. It takes a cellSet and creates a whole new fvMesh from it and subsets the cells as well.

Ok, new questions... In the s
 

Ok, new questions...
In the subsetMesh utility the following lines read the mesh and the volume scalars from a specific time directory:

IOobjectList objects(mesh, runTime.timeName());
wordList scalarNames(objects.names(volScalarField::typeName ));
PtrList<volscalarfield> scalarFlds(scalarNames.size());

then a subset of it is constructed by

subsetVolFields(subsetter, scalarNames, scalarFlds);

Now my question is: how do I construct the subset from the variables I have in memory (during the calculation) and not read them from a dictionary?

Dragos

wiki: TurbPlaneCutFoam
 

wiki: TurbPlaneCutFoam

Hmm, I need an idea: how to ma
 

Hmm, I need an idea: how to make it run in parallel?
Anybody can give me a clue?
This is the log file with the error I get when I run the solver in parallel:
http://www.cfd-online.com/OpenFOAM_D...hment_icon.gif channel_par.log

Dragos

Hello again, Running in paral
 

Hello again,
Running in parallel and getting the slices saved, seems to be ok. But how should I reconstruct the plane back from each processor? For instance, two processors will give me two pieces like in the following image:
http://www.cfd-online.com/OpenFOAM_D...ges/1/6593.png
How should I put them together?
reconstructPar doesn't seem to work for the cells saved from the cuttingPlane.
I can merge the mesh using mergeMeshes, but how can I merge the data?

Dragos

Hi Dragos, I tried your cod
 

Hi Dragos,

I tried your code snip, but have some problems compiling it:

-lincompressibleLESmodels -lincompressibleTransportModels -lfiniteVolume -lmeshTools -lOpenFOAM -liberty -ldl -lm -o /home/gcae504/OpenFOAM/gcae504-1.4.1/applications/bin/linux64GccDPOpt/no_avg_ood les
Make/linux64GccDPOpt/no_avg_oodles.o(.text+0x31b5): In function `main':
: undefined reference to `Foam::cuttingPlane::cuttingPlane(Foam::primitiveM esh const&, Foam::plane const&)'
Make/linux64GccDPOpt/no_avg_oodles.o(.text+0x31c2): In function `main':
: undefined reference to `Foam::cuttingPlane::cells() const'
collect2: ld returned 1 exit status
make: *** [/home/gcae504/OpenFOAM/gcae504-1.4.1/applications/bin/linux64GccDPOpt/no_avg_oo dles] Error 1

I added these libraries to the oodles solver:

#include "plane.H"
#include "cuttingPlane.H"
#include "cellSet.H"
#include "fvMeshSubset.H"

Would be nice, if you have a hint, how to compile it!?

Regards!
Fabian

Hi Fabian, It seems that you
 

Hi Fabian,
It seems that you have all the correct "#include" directives, since the error is from the link stage and not from compilation. What you basically need is the "-lsampling" option. Here is how my options file looks like:

EXE_INC = \
-I$(LIB_SRC)/LESmodels \
-I$(LIB_SRC)/LESmodels/LESdeltas/lnInclude \
-I$(LIB_SRC)/transportModels \
-I$(LIB_SRC)/finiteVolume/lnInclude \
-I$(LIB_SRC)/meshTools/lnInclude \
-I$(LIB_SRC)/sampling/lnInclude

EXE_LIBS = \
-lincompressibleLESmodels \
-lincompressibleTransportModels \
-lfiniteVolume \
-lmeshTools \
-lsampling